A hydrostatic pressure load simulates pressure that occurs due to fluid weight.
Hydrostatic Pressure is available for the following analysis types:
This section describes the characteristics of the boundary condition, including the application requirements, support limitations, and loading definitions and values.
Dimensional Types
3D Simulation: Supported.
2D Simulation: Supported.
Geometry Types: Geometry types supported for the Hydrostatic Pressure boundary condition include:
Solid: Supported.
Surface/Shell: Supported.
Wire Body/Line Body/Beam: Not Supported.
Topology: The following topology selection options are supported for Hydrostatic Pressure.
Body: Not Supported.
Face: Supported (3D).
Edge: Supported (2D).
Vertex: Not Supported.
Nodes: Not Supported.
Loading Types: The boundary condition’s loading is defined using one of the following options.
: Supported.
The vector load definition displays in the Annotation legend with the label Components. The Magnitude and Direction entries, in any combination or sequence, define these displayed values. These are the values sent to the solver.
: Supported.
Loading Data Definition : Hydrostatic Pressure is defined as a constant.
Note: During a multiple step analysis, tabular data is visible for this boundary condition. This information is read-only but you can use the context menu (right-click) features of the Tabular Data display to activate or deactivate the loading per step.
To apply a Hydrostatic Pressure:
On the Environment context toolbar: click Loads>Hydrostatic Pressure. Or, right-click the Environment tree object or the Geometry window and select Insert>Hydrostatic Pressure.
Define the Scoping Method. Hydrostatic Pressure can only be scoped to faces.
Select all of the faces that will potentially enclose the fluid.
Or...
If you are working with a surface body, specify the Shell Face, defined as the side of the shell ( or ) on which to apply the hydrostatic pressure load.
Specify the magnitude and direction of the Hydrostatic Acceleration. This is typically the acceleration due to gravity, but can be other acceleration values depending on the modeling scenario. For example, if you were modeling rocket fuel in a rocket’s fuel tank, the fuel might be undergoing a combination of acceleration due to gravity and acceleration due to the rocket accelerating while flying.
Enter the Fluid Density.
Specify the Free Surface Location, defined as the location of the top of the fluid in the container. You can specify this location by using coordinate systems, by entering coordinate values, or by clicking a location on the model.
Mesh the model, then highlight the Hydrostatic Pressure load object to display the pressure contours.
The following example shows the simulation of a hydrostatic pressure load on the wall of an aquarium. Here the wall is modeled as a single surface body. The load is scoped to the bottom side of the face. A fixed support is applied to the bottom edge. Acceleration due to gravity is used and the fluid density is entered as 1000 kg/m3. Coordinates representing the top of the fluid are also entered.
The load plot shown here illustrates the hydrostatic pressure gradient.

The selections available in the Details view are described below.
| Category | Fields/Options/Description |
|---|---|
| Scope |
Scoping Method, options include:
|
| Definition |
: Read-only field that displays boundary condition type - Hydrostatic Pressure. Coordinate System: Drop-down list of available coordinate systems. is the default. Suppressed: Include ( - default) or exclude () the boundary condition. Fluid Density: Input field for fluid density value. |
| Hydrostatic Acceleration |
Define By, options include:
|
| Free Surface Location |
X Coordinate Y Coordinate Z Coordinate Location: Specify Free Surface Location using geometry picking tools. Valid topologies include: face, edge, vertex. |
The following Mechanical APDL commands, element types, and considerations are applicable for this boundary condition.